xSignals Multi-Chip Wizard

Now reading version 20.0. For the latest, read: xSignals Multi-Chip Wizard for version 22

The opening page of the xSignals Multi-Chip Wizard
The opening page of the xSignals Multi-Chip Wizard


The xSignals Multi-Chip Wizard is used to create xSignals between a single source component and multiple target components. The Wizard uses a component-oriented approach to identifying potential xSignals – you select a single source component, the nets of interest and the target components and the Wizard then analyzes all potential paths from the source component to the designation components, passing through series passive components and along any branches. As the designer, you then can choose the xSignals you would like to have generated and you can also create Matched Length design rules if required. The Wizard also can be used to automatically create xSignals and xSignal classes for a number of different common interface and memory circuits.

 In this Wizard, an output pin is referred to as the Source, and the target input pin is referred to as the Destination.

The Wizard is also a multiple-run tool – from the overall master group of xSignals that you initially create on the xSignal Routes page, you can select a sub-set of these, define classes and rules, then return to the master group, choose another sub-set, define classes and rules for them, and so on.

One of the great strengths of the Wizard is the ease of working between the Wizard and the PCB editor. Click on an xSignal on any page of the Wizard and the pads and any routing are visually highlighted on the PCB.

At this stage, the Wizard does not support the automatic addition of T-junction identifiers, often referred to as tie-points or branch-points. If your design includes branched routing, it is suggested that you:

  1. Tune the length from the source component to the passive component (such as a series termination resistor), if there are any.
  2. Tune the length in each branch, from the T-Junction to the destination component.
  3. If required, tune the remaining length between the passive component (or from the source if there are no passives) to the T-junction.
If you need to tune the lengths of just the branches, create a user-defined branch point by placing a single-layer, single-pad component within the routing at the T-junction. Refer to the Defining the Branch Point in a Balanced T Pattern topic in the Defining High Speed Signal Paths with xSignals page for more information.


With a PCB open as the active document, the xSignals Multi-Chip Wizard can be launched in the following ways:

  • Click Design » xSignals » Run xSignals Wizard from the main menus.
  • Right-click in the PCB layout and then select xSignals » Run xSignals Wizard.


Wizard Navigation

  • Click Cancel to close the xSignals Multi-Chip Wizard​.
  • Click Back to navigate to the previous screen.
  • Click Next to navigate to the next screen.
  • Click Finish to close the xSignals Multi-Chip Wizard

xSignals Multi-Chip Wizard Modes

On the second page of the Wizard, you will be asked to select either Custom Multi-Component Interconnect, On-Board DDR3 / DDR4, or USB 3.0. The Custom Multi-Component Interconnect mode is used to define multiple xSignals between a chosen source component and multiple target components, while the On-Board DDR3 / DDR4 mode is used to create xSignals for your DDR3 or DDR4 memory. The USB 3.0 mode creates the xSignals, xSignal Classes, and Matched Length rules for each USB 3.0 channel. Select the appropriate mode for your needs

Click the link below that corresponds to your selection for information about that mode

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

The features available depend on your Altium product access level. If you don’t see a discussed feature in your software, contact Altium Sales to find out more.